Impedance control in antenna line - PLS62-W | Thales IoT Developer Community
July 25, 2019 - 4:56pm, 5003 views
I am developing a new application board to fit in our requirements, and I am stuck in the antenna impedance.
I was using the PLS8-US_HD_v01.000c given in https://iot-developer.thalesgroup.com/documentation/pls8-us-technical-documentation, which seems to be the same family of PLS62-W.
In section 4.1.2.2 recommends to use a Stripline (50 Ohms) under the module, and out of the module it recomends a Microstrip (50 Ohms). It makes sense once the module and the reference ground makes a ground "sandwich" in the antenna line.
Analysing the Figure 17 (PLS8-US evaluation board layer table), the third layer seems to be the reference, so:
- Substrate Height 1: 798 (708+25+65)um,
- Trace Thickness: 25 um,
- Substrate Height 2*: +/- 40um (two green coat),
- Trace Width: 330 um,
-Substrate Dielectric: 4.4 (it was considered that substrate 2 has the same dielectric as substrate 1 - probably wrong).
With this considerations and values, I could get 50 Ohms strip line, but I do not feel safe to use it in my application board, because the layer table is different.
I would like to know what parameters (Substrate Height 2 and Substrate Dielectric2) were used to calculate the stripline 50 Ohms?
I've seen this, it's a terrible problem. I also have the same problem here, as the documentation causes questions and leaves us without understanding, 65 ohms under the module, 50 ohms outside, but with what?
There is no right point of reference, you can't be sure that the third layer is the point of reference, so I think it's a flaw in their documentation. Very sad this!
We are also having difficulty on this point.
Hello,
PLS8 is a different module. You should be using the documentation for PLS62. Please see this link and find hardware description document for your module:
https://iot-developer.thalesgroup.com/documentation/download-documentati...
This chapter shows an example only - have you tried to use the software from previous chapter or any other for calculations? At the moment I don't have any HW expert for a fast consultation in my office.
Regards,
Bartłomiej
Hello Bartłomiej,
We do not have the polaris calculator, and the AWR calculator do not have the Asymetric Strip line, so we used this calculator:
http://mark-hoffman-eng.com/zocalc/pages/fmas.html
The figure attached shows the parameters that we have used to get closer to 50 Ohms impedance under the PLS62-W module. Those parameters were extracted from example in the section 2.2.3.2 from file pls62-w_hd_v02.000b.pdf.
Considering the antenna is traced in the top and its reference is the bottom in the applacation board, the bottom dielectric is 888 micrometer (um), the width is 330um, dielectric of 4.4 dielectric.
The top height would be the space from top application board to the bottom of PLS62 module, considering that is "air" (dielectric would be 1), to get closer to 50 Ohms, the top height is 90um.
As shown in the figure below:
Thanks and Regards,
Willian
Hello !
We will check that topic internally with our hardware expert and let you know.
Best Regards
Wojciech
Hello,
I have consulted a hardware college - if you still have this problem please send me a layer stackup of your PCB and we can calculate the paths parameters.
We can also advice KiCad program which has a quite nice calculator or you can use this site: https://www.eeweb.com/tools/asymmetric-stripline-impedance
As for your calculations you have used an asymmetric stripline calculator while you said about antenna on the top of PCB and you also mentioned air. It is important to use the right calculator. It could be "coplanar wave guide with ground plane" (RF on the surface with ground on both sides and underneath) or "microstrip line" (RF on the surface with the ground undeneath only) or "stripline" (RF in the middle layer with a ground on the top and bottom of it).
Best regards,
Bartłomiej
Hello Bartłomiej and Wojciech,
Thanks for your support!
The stack layer that we are using is:
Top Layer: 18 um + 22 um (plating);
Dielectric 1: 117 um (FR-4 1080);
Layer 2: 35 um;
Dielectric 2: 610um (FR-4 1080);
Layer 3: 35 um (reference);
Dielectric 3: 117um (FR-4 1080);
Bottom Layer: 18 um + 22 um (plating);
I was calculating with asymetric stripline while the antenna is under the module and out of the module I used Coplanar Wave Guide with Ground Plane, and we get the following design:
Best Regards,
Willian
Hello,
According to the hardware expert your calculations out of the module are OK.
Under the module there is only a 2mm path so there's no harm even if your values would differ by a few Ohms from the ideal ones.
Best regards,
Bartłomiej
Hello Bartłomiej,
OK, That is good to hear that is fine!
Thanks and Best Regards,
Willian